Using Clever Techniques to Convert a Passive Audio Filter Into an Active Filter

Previously, I introduced a design for a ‘468-4’ audio filter, which implements a standardized noise measurement that approximates subjective assessments of people listening to music and talking.

As discussed in that article, there are two primary ways of making an active filter that provides the 468-4 frequency response and matches the impedance levels of modern audio equipment:

1. Merge conventional low and high-pass active filters around 6.3 kHz.
2. Derive an active circuit from the passive circuit using clever mathematical techniques.

I previously covered the first method, and now this article will cover the second method.

The Original 468-4 Passive Filter Design

As a quick refresher, the network of Figure 1 was developed in the 1950s to provide the desired frequency response for use in audio systems with 600 Ω impedance.

Figure 1. Passive network implementation of the 468-4 filter for 600 Ω circuits (click to enlarge).

The source and load resistors are shown at left and right, respectively, but there is no signal source. This circuit requires an amplifier at the output to compensate for its significant insertion loss.

Impact of Inductor Resistance

The frequency response for the specification was likely determined by measuring the original network, which is affected by the losses in the inductors.

The specification requires that inductor Q factors exceed 200 at 10 kHz, but that is not a sufficient specification for two reasons:

1. The inductors have series resistance and (if not air-cored) parallel loss resistance, but we do not know how much of each resistance.
2. The parallel loss is frequency-dependent, so it cannot be fully modeled by a fixed resistor.

Investigation of the inductors shows that, with the lowest permissible inductor Q of 200, the distribution of loss between series and parallel resistance makes very little difference to the frequency response, even in the critical 6 kHz to 14 kHz range. This is also true for ideal inductors with no resistive losses. For parallel capacitances to have any effect, they would have to be in the nanofarad range, which, of course, they are not.

Impact of Capacitor Variation

The specification also states that the value of the 33.06 nF capacitor may need adjustment to meet the specified tolerance limits for the frequency response. I have investigated these effects using an LTspice simulation. The impact of varying the 33.06 nF capacitor by ±5% was negligible (microbels!).

Simulating the Effects of Component Variation

In simulation, we can vary the components across their tolerance limits of ± 5%. The frequency responses of all the network variants are plotted in Figure 2, with the specification limits highlighted in yellow.

Figure 2. Varying the component values has little effect on the frequency response of the passive network 468-4 audio noise filter (click to enlarge).

As illustrated in Figure 2, the frequency response does not change much as a function of the component tolerances, and all variants meet the specification.

Beware of Interpolation

However, you may notice the strange hump in the frequency response curves of Figure 2 centered near 11 kHz. This hump was also seen in the simulations and measurements in the previous article. It looks like a data error, but the data is correct.

The cause is the large step from 10 kHz to 12.5 kHz in the frequency response specification, which I replicated in the simulation. This large 8.1 dB step in the frequency step simulations forces the simulation plotting tool to interpolate the data to draw the curves.

Linear interpolation between 10 kHz and 12.5 kHz gives a response at 11 kHz of 4.63 dB, whereas all the simulated networks have a response very close to 5.30 dB. If we add additional frequency steps into the simulation, that blip at 11 kHz has nearly vanished, as shown in Figure 3.

Figure 3. Adding additional frequency steps reduces interpolation and removes the hump in the response curves (click to enlarge).

The remaining humps and dips are due to rounding effects in the frequency response specification. For this reason, it is better to compare the results of the constructed and measured filter with the frequency response of the simulated passive network, both of which have very small rounding errors.

Turning the Passive Network Into an Active Network

It’s pretty well known that you can ‘scale’ any RLC network by dividing all component impedances by a fixed scale factor. The frequency response does not change as long as the source and load impedances are included in the calculations.

In 1968, Leonard Bruton demonstrated that the Bruton Transform process still works if the scale factor is imaginary (one that includes j, the square root of minus 1). It works particularly well if we include the angular frequency, ω:

$$\omega = 2 \pi f$$

Equation 1.

where:

f is the frequency in hertz.

Scaling Inductors by an Imaginary Angular Frequency

We will divide all of our components by the scale factor jω. Let’s start by examining the change for an inductor with impedance jωL.

$$\frac{j \omega L}{j \omega} = L$$

Equation 2.

Don’t be fooled by the use of the term L. This impedance is independent of frequency, which means it is a resistor with a resistance value of L. Replacing an inductor with a resistor in our circuit will provide a cost-saving!

Scaling Resistors by an Imaginary Angular Frequency

Now, let’s see what happens when we divide a resistor by the scale factor jω.

$$\frac{R}{j \omega} = \frac{1}{j \omega (\frac{1}{R})}$$

Equation 3.

This changes our resistor into a capacitor with a capacitance value of (1/R). You may recognize this value as the conductance, G, of our original resistor.

Scaling Capacitors by an Imaginary Angular Frequency

Finally, let’s divide the impedance of a capacitor by our scale factor jω.

$$(\frac{1}{j \omega C}) \cdot (\frac{1}{jw}) = -(\frac{1}{\omega^2C})$$

Equation 4.

That result doesn’t look very promising. It’s a mathematically real impedance (no ‘j’ there), with voltage in phase with current, like a resistor, but it’s negative and frequency-dependent.

It can be called a frequency-dependent negative resistor (FDNR), or a ‘D-element.’ This is an active component that supplies energy to an ordinary resistor, so it needs a power supply. Luckily, it can be built from opamps, resistors, and capacitors.

Using Duality To Transform a Circuit Schematic

If we refer back to Figure 1, we see that C3 isn’t grounded at either end. This will create a real problem when it’s converted to a D-element because that would need a floating power supply. Before we do our Burton Transform, we can overcome the C3 issue with another mathematical trick and the duality property of electrical circuits.

In this process of “dualling,” we can transform a schematic by making the following changes.

• Voltage source ↔ current source
• Inductance ↔ capacitance
• Resistance ↔ conductance
• Series ↔ parallel

Inductances and capacitances change their nature–the way they store energy and how their impedances vary with frequency. Resistances and conductances do not change their nature, so we can regard them in either form without introducing error.

The numerical values of the components do not change, although the result may include impracticable values (but that can be fixed later). The resulting schematic will have the same frequency response.

If we apply the dualling process to the 468-4 filter circuit of Figure 1, we must include the source and load resistors. These resistors are converted from 600 Ω to 600 S (siemens) conductances, which is equivalent to a 1.667 mΩ resistor.

Completing our dualling conversion on the 468-4 filter circuit results in the new schematic shown at the bottom of Figure 4. I have replicated the original circuit at the top of Figure 4 so you can see the dualling transformation more easily.

Figure 4. Original 468-4 audio noise filter (top) and the dual passive network version (bottom) (click to enlarge).

Obviously, with component values in the nanohenrys, milliohms, and millifarads, this is a very low-impedance network. Not to worry, we can fix that!

Scaling Components Values With the Bruton Transform

Now, we come to another clever bit: converting the component values using the Bruton Transform. We can introduce a new factor to scale all the component values to something much more convenient.

We will start by converting the 1.667 mS source and load conductances to a reasonable capacitor size of 1 nF. As introduced earlier, the Bruton transform converts a resistor to a capacitor using the following equations:

$$\frac{R}{j \omega} = \frac{1}{j \omega G} \rightarrow \frac{1}{j \omega C}$$

Equation 5.

Now, let's calculate our scale factor:

$$\text{Scale Factor} = \frac{C}{G} = \frac{1\text{ E-9}}{1.667\text{ E-3}} = 6.0 \text{ E-11}$$

Equation 6.

Don’t worry that it’s an extremely high number; it’s just a scale factor.

• Divide resistor values by the scale factor to get the capacitor values (equivalently, multiply conductance values by the scale factor).
• Divide capacitor values by the scale factor to get the D values.
• Multiple inductor values by the scale factor to get the resistor values.

Figure 5 is our circuit after completing the Bruton transformation on all circuit elements.

Figure 5. Network after the Bruton transform, including the D-elements (click to enlarge).

There isn’t a standard unit name for the D-element, but we’ll just call it the bruton and give it the symbol Br. Our resulting D values are in femtobrutons, but never mind. We can make them from opamps, resistors, and capacitors using sensible component values. Note that their impedances are just negative resistors with frequency-dependent values in ohms.

Generalized Impedance Converters for Negative Resistors

We will create our D-elements using Generalized Impedance Converters (GICs). The explanation of how they work is rather long and mathematical (simple math, but a lot of it).

The GIC schematic is shown in Figure 6. 

Figure 6. Generalized impedance converter schematic.

The impedance Z between the GIC terminals is given by the formula:

$$Z = \frac{Z1 \times Z2 \times Z3}{Z2 \times Z4} $$

Equation 7.

We need a GIC with two capacitors and three resistors in the series chain, as shown in Figure 7.

Figure 7. Final D-element schematic with component values (click to enlarge).

We have again chosen the convenient value of 1 nF for capacitors C1 and C2. Likewise, R1 and R2 are selected at 10 kΩ (another convenient value).

The R3 values must be calculated to give the right value for the two D-elements in our schematic of Figure 6, using:

$$R3_1 = \frac{D_1}{C1 \times C2} = \frac{21.47 \text{ E-15}}{1 \text{ E-9} \times 1 \text{ E-9} } = 21470 \text{ } \Omega $$

Equation 8.

and

$$R3_2 = \frac{D_2}{C1 \times C2} = \frac{44.15 \text{ E-15}}{1 \text{ E-9} \times 1 \text{ E-9} } = 44150 \text{ } \Omega $$

Equation 9.

Our resulting R3 values are of the same order of magnitude as R1 and R2.

Simulating our Filter Design with LTspice

We can now use LTspice to simulate our filter to check that it works as expected. Figure 8 shows the LTspice schematic, in which I have also included the passive filter as a reference.

Figure 8. LTspice simulation schematic of the 468-4 audio noise filter (click to enlarge).

The schematic shows the exact values for the resistors, which can be made from series or parallel combinations of E12 ±1% tolerance resistors. I am using TL07x op amps for this simulation.

This type of filter implementation is claimed to be more tolerant of component values than implementations using conventional filter sections. However, that is far too complex an issue to go into here.

Figure 9 shows the result of the simulation.

Figure 9. Deviation of the simulated response from the 468-4 audio noise filter reference and the specified tolerances (click to enlarge).

Clearly, the result is very good up to 10 kHz and remains within the lower tolerance up to 31.5 kHz, but it does droop. This is due to the op-amps' limited bandwidth. Better results can be obtained with faster op amps, such as NE5532, but these require more supply current.

A Warning About Circuit Stability

Ultimately, I settled on using LM4562 op amps for the hardware design (as I will show below). When using much faster op amps, there is a real risk of one of the GICs becoming unstable due to the complex closed-loops configuration.

When using any Spice or similar simulation tool, it is strongly advised to run a time-domain simulation (called .TRAN in Spice) in addition to the frequency-domain sweeps (.AC in Spice). The .AC frequency simulations cannot detect the oscillation. A good indicator of internal oscillation is that the .TRAN simulation runs very slowly.

The Final Test: Building the 468-4 Audio Noise Filter

The critical test is building the filter in the real world and measuring its performance. Figure 10 shows the hardware schematic used as an add-on for my previous Wideband Voltmeter project.

Figure 10. Schematic of the 468-4 audio noise filter using LM4562 op amps (click to enlarge).

This design includes the same gain adjustment circuit as demonstrated in the previous audio noise filter design. However, this filter's range of gain variation is expected to be small.

Figure 11 shows the real circuit's frequency response compared with the passive circuit's simulated response. Deviations are only just detectable and are small fractions of a decibel. Success!

Figure 11. Simulated passive and measured active audio noise filter responses (click to enlarge).

That’s all of the filters for now. It's time for me to work on something different.

Author’s acknowledgment: I am very grateful to Kendall Castor-Perry for helping me design the filter for this project.

Featured image used courtesy of Adobe. All other images used courtesy of the author.